mirroring sheet metal parts

[bnemec]

Using the Insert -> Mirror Part... method to create a mirrored part in a new file, with no context ref to an assembly. On some parts we need to make small edits to the part for laser cutting, removing chamfered holes, adding material for an edge that needs machined tolerance, adding a little divot to indicate laser start/stop for example. We do these operations in the Default config (not using any other configs than the automatic one for flat view on drawing) and after the Flat-Pattern feature. This way they formed model looks correct in assemblies and drawing view, but the dxf is also correct with chamfers removed, etc.

Now to the mirroring part. I cannot understand how SW mirrors a part. What it choses to copy and ignore. I do not see a way to get it to bring the flat pattern with, so it seems like all it does is mirror the dumb geometry and make DerivedBends so it has something to flatten, as well as the file properties per the mirror dialog checkboxes. Is there a good, robust way to get it to mirror the features we add after the Flat-Pattern feature? Currently we go add them again in the mirrored file, which is a bit of a struggle for some to understand why they need to do that. Also on edits people forget to go edit the post-flat features in the mirrored file. So we already have a hack work around, just looking for something less hacky I guess.

Thanks.

[DLZ_SWX_User]

Hello,

I see that no one has responded to your question. I had a similar issue a while back & my VAR told me that I have to add that feature into the mirrored part! There was a thread a while back discussing hole wizard info & a mirrored part: viewtopic.php?t=2708

Not sure if this helps or not. I do know this that the longer I use SolidWorks the more I discover that it does not always behave the way I think it should.

[bnemec]

Hello,

I see that no one has responded to your question. I had a similar issue a while back & my VAR told me that I have to add that feature into the mirrored part! There was a thread a while back discussing hole wizard info & a mirrored part: viewtopic.php?t=2708

Not sure if this helps or not. I do know this that the longer I use SolidWorks the more I discover that it does not always behave the way I think it should.

Thanks. I was assuming it was such a bad question that it wasn't worth responding to. Not sure if anyone else adds features (like cut or delete face) after the Flat-Pattern feature. The other thread does help a little, mostly to add uncertainty to the various forms of mirroring operations.

The longer I use Solidworks the more it feels like everything is an afterthought, implemented to about 90% of completion, that must be made to fit around all of the previous 90% implemented afterthoughts. I thought Solid Edge was frustrating to use, now I'm having afterthoughts....

[TTevolve]

I do a bunch of sheet metal parts where I need a right hand /left hand parts, and I always end up making each from scratch. I have never had good luck trying to mirror parts. Most of what I do sheet metal wise is fairly simple so making a opposite hand is not to difficult. To me, the extra amount of time taking to model it separately vs. mirroring a part is worth it to keep my sanity.

Plus it almost never fails that we will add holes or other cuts on the mirrored part that won't be in the original part.

[DLZ_SWX_User]

Plus it almost never fails that we will add holes or other cuts on the mirrored part that won't be in the original part.

And then after you do that minor change, awhile later, "we need this hole/cut/bent flange on the original but moved just a fraction". Especially since a lot of or work done here is custom one off items.

[Dwight]

. . . I always end up making each from scratch. . . .

I assume you'd copy the left hand part file and edit the tree to make it a right hand part.

Dwight

[TTevolve]

I assume you'd copy the left hand part file and edit the tree to make it a right hand part.

Dwight

Yea, most times a "save as copy" works well and then reverse the bends. Knowing how to do cuts and holes past the bends on the tree so they don't blow up on you takes some experience.

[Bryan O]

I'll start with "I don't use sheet metal much, but when I do..."
I remember in previous version that mirroring was a No No.

I recently had the same issues.
I'll give you the technique I use for "regular" solid handed parts which seemed to work in this case.

Last feature in the tree is a Mirror Body -> Delete Body to create my handed part.
For the NON handed I suppress the feature in that configuration.
Any changes to either part requires a roll back before the Mirror Body -> Delete Body and then end by rolling the tree forward.
Any "Hand specific" feature is on or off in that configuration.
I could not select either the main plane or a surface on the part to mirror about so I had to create a reference plane.

I always let SW create the Flat Pattern for the drawing views.

Attached is a copy of a part that I helped someone with.
Disclaimer - I didn't create this part so I take no create for any of the techniques used beyond what I described above.